PDA

View Full Version : Drilling and tapping 200 4-40 holes



Magee
06-09-2010, 10:01 AM
Hello gents,
First, I KNOW I have seen this topic come up before, but couldn't manage to dig it up with many attempts at a search, so apologies for digging up and beating a dead horse.

I've been asked to drill and tap 200 4-40 holes in a small extruded aluminum heatsink. The holes will be between the fins and as such can go all the way through the part. I have a Bridgeport with a DRO, so locating the holes is no biggie...
Any advice?
I do not have a tapping head for what it's worth.

Can I use a DRAP on the mill?

It seems like the job isn't worth my time if I have to locate, spot, drill then tap X 200.

Thanks.

http://www.heatsinkusa.com/Displayfile/index.aspx?storename=heatsinkusa&manip=&table=template_options&icol=image2&tcol=image2_content_type&id=Home

SGW
06-09-2010, 10:09 AM
Without CNC, I think I'd make a fixture to hold the part, then drill all 200 of the first hole, then reset the fixture and drill all 200 of the 2nd hole, etc. Then go back and tap the 4th hole (since the fixture would be set for that position), reset and tap another hole, etc.

If you use a split-point drill, you probably wouldn't need to spot first. I also think I would drill from the back, if possible.

It could get pretty tedious.

mochinist
06-09-2010, 10:16 AM
A tapping head would make things faster, but without one you can just tap under power, holding the tap in the drill chuck. Personally I would use a roll form tap for this job, and it should really be done on a cnc to make it affordable.


Can I use a DRAP on the mill? :confused: It will probably seem obvious when someone say's it, but what is DRAP?


It seems like the job isn't worth my time if I have to locate, spot, drill then tap X 200.If you can spot, drill and tap the holes at a minute a piece average you are looking at almost 3.5hrs of work.

I don't know what your shop rate is or what your customer is willing to pay, and lastly what your time is worth, so it is hard to say.

Magee
06-09-2010, 10:22 AM
:confused: It will probably seem obvious when someone say's it, but what is DRAP?

Combination Draill/tap. Beyond being aware of their existence, I have a grand total of 0 experience with them.
http://www.use-enco.com/ProductImages/8272440-11.jpg



If you can spot, drill and tap the holes at a minute a piece average you are looking at almost 3.5hrs of work.

I don't know what your shop rate is or what your customer is willing to pay, and lastly what your time is worth, so it is hard to say.

Yeah, that's the big question. I'm not doing this full time, so it comes down to what small amnout of money makes it seem worthwhile, even on a psychological level so I don't end up inventing new curse words 1/2 way through the job :D

Evan
06-09-2010, 10:25 AM
Ask what alloy the heat sink is made from. Heat sinks are frequently made of 1100 series alloy for best heat conduction. If that is the case then give it a pass since 1100 alloy is miserable to machine because it is so soft. If it is 6061 then what you need is a drilltap.

http://ixian.ca/pics7/drilltap.jpg

http://www.alfatools.com/cat2/main18.pdf

Magee
06-09-2010, 10:31 AM
Thanks for the tip Evan.
So what's the preferred method for using one of these drap numbers on a manual mill?
Just quill feed by hand, under power?

Tony Ennis
06-09-2010, 10:37 AM
Perhaps OT, but why does this need 200 holes? That's a lot of holes.

Evan
06-09-2010, 10:37 AM
I don't know. My mill is CNC. Another item. If the heat sink is already anodized it will eat your tooling for lunch. Anodized heat sinks have a much thicker layer than decorative anodizing and that layer is as hard as sapphire. In fact, it is a form of sapphire.

airsmith282
06-09-2010, 10:46 AM
id agree with evan on the use of the drilltap but make sure the type of metal and if it was anodized or not , but even if it was you still might be ok id think, i dont know alot about the anodizing process my self, but a drill tap does make sence and is alot faster to do then the old fashion way,,

George Bulliss
06-09-2010, 10:59 AM
This job is almost identical to one I worked on. Itís been over ten years, so Iím a little unsure of all the details but the heat sink was almost identical looking and the holes were also 4-40. I canít remember the total number of holes but it was a ridiculous amount, well over 100.

Anyway, we did about 30 of them on a CNC and never did get the cycle time down to where we made a profit. As Evan suggested, the aluminum turned out to be gummy and we went through a number of taps. We tried different styles of taps but never tried a DRAP. I would think that unless your material was clean cutting you would have trouble getting the drill and tap to work well at the same rpm. A speed change on a CNC is fairly simple but it may take you more time on your mill than a tool change.

George

hitnmiss
06-09-2010, 11:09 AM
My no actual experience answer to the "if it's gummy al" problem would be to try a roll (form) tap.

Actually I'd try a roll tap no matter what cause they don't cut chips you have to clean...

fasto
06-09-2010, 11:33 AM
Magee if you end up in a bind drive 35 miles West on Rt 9 and we can slap it on my VMC.
Otherwise, having done a number of these on a manual mill with DRO, I'd:
1) Get a #1 Procunier tap head.
2) Get a collection of #4-40 draps.
3) Dial up 500 RPM or so.
4) Shoot each hole right through. Yes, drill with the tapping head. Pause after breaking through to blow the chips off, before hitting it with the tap. Replace the drap immediately it starts getting dull.
5) Use a thin Scotch-Brite EXL deburring wheel to go down between the fins & clean up the burr.

If you want to borrow a Procunier I have some #1 and #2 heads.

If you don't want to do that,
1) Get a screw machine length tap drill drill. Chuck the drill as short as you can to minimize how much it flexes. Chuck on the flutes, if you must.
2) Use a #1 Procunier head, set up with a #4-40 roll form tap.
3) Drill all 200 holes.
4) Tap all 200 holes.
4) Use the EXL deburring wheel.

I wouldn't attempt to change the part & reclamp after each hole. Even if you've only got 2 parts, that's 400 clamp cycles, which is going to take 3-ish hours of your total time.
I wouldn't attempt to do a toolchange between each drill/tap operation. That's going to take absolutely forever.
--
Aaron

becksmachine
06-09-2010, 01:16 PM
If you can do this from the back side, you don't need to do the through drilling, or tapping operations in a mill.

#1 Do a spot drill operation on all 200 holes.

#2 Go to your favorite high speed drill press and drill all 200 through holes by manually moving the piece on the drill press table. It helps to have a table that isn't full of holes. ;)

#3 Set up the tapping head and then tap all holes using the same method. A roll form tap works good in aluminum.

This was the method of choice for castings for Hewlett Packard that came with a dimple already cast into the part. I have done tens of thousands of holes like this.

Dave

Paul Alciatore
06-09-2010, 01:39 PM
One thing I have done when I had to tap a large number of holes in copper, which is also gummy, was to use a battery powered hand drill for the tapping. It actually goes a lot faster than either drill press or mill. But it does take a bit of skill in making the holes square. You would want a drill model that has a slow speed and an easy reverse mechanism.

It would go something like this:

1. Drill the holes using whatever method is best for locating them properly.

2. De burr if needed.

3. Place some cutting fluid (WD-40 for aluminum?) in a cup, about 1/2" deep.

4. Chuck the tap tightly in the drill.

5. a. Dip tap in cutting fluid
.....b. Tap hole in one motion
.....c. Reverse the drill to extract tap
.....d. Switch to forward and repeat from 5a until all holes are tapped.

I don't have any experience with a form tap so I would probably use a spiral point to push the chips ahead of it.

If chips are accumulating on the tap, you can put a brush on the bench (in a vise?) and just draw the rotating tap through it to clean it.

It would probably go faster if the heat sink was mounted in a vise, vertically for easy access.

You can probably do several holes a minute using this method. Dip - tap - reverse - clean - repeat. If you have multiple pieces you may need several battery packs and extra chargers.

Magee
06-09-2010, 04:35 PM
Thanks for all of the tips and big thanks to Aaron for that offer. Top Notch.
It's looking like I'm going to pass on this job. In my back-and forth with him I think this guy was thinking I could magically make it happen for $20 or something. I just don't think he gave a whole lot of thought to how long it would take a human to pull it off.

fasto
06-09-2010, 04:53 PM
I could magically make it happen for $20
He's only off by a factor of 10... :D

mochinist
06-09-2010, 05:13 PM
Thanks for all of the tips and big thanks to Aaron for that offer. Top Notch.
It's looking like I'm going to pass on this job. In my back-and forth with him I think this guy was thinking I could magically make it happen for $20 or something. I just don't think he gave a whole lot of thought to how long it would take a human to pull it off.welcome to the world of machining for money:p

becksmachine
06-09-2010, 07:48 PM
Thanks for all of the tips and big thanks to Aaron for that offer. Top Notch.
It's looking like I'm going to pass on this job. In my back-and forth with him I think this guy was thinking I could magically make it happen for $20 or something. I just don't think he gave a whole lot of thought to how long it would take a human to pull it off.

I agree that is unreasonable for a one of, but not that far off in production quantities. Back when I was working on those HP parts, the rule of thumb was a nickel a hole. Now I can't remember if that was for a drilled and tapped hole or a nickel for drilling the hole and an additional nickel for tapping, but as primitive as the process may seem, it was fast.

Dave

squirrel
06-09-2010, 10:49 PM
You can run a tapmatic on the CNC and will be smoking fast, use a short solid carbide and plenty of coolant for the pilot. It really boils down the cost, our Haas has a digital spindle control and it does and excellent job with 4-40's I was shocked the first time ridgid tapping a 4-40, the older analog machines would be tricky with 8-32's. Also use a spiral tap to clear out the chips.